Modernize Mold Using CNC Technology

• 1
  What changes when you modernize mold using CNC technology
• 2
  5-axis machining and where it earns its place on mold work
• 3
  Setup strategy, stock allowance and in-process probing
• 4
  Tool steel selection and the heat-treat window
• 5
  Surface finish, polishing allowance and texture
• 6
  What the shop needs to run this kind of mold work
• 7
  Choosing a machining approach for each mold feature

A mold is a stack of plates, inserts and cores that must close on a common datum thousands of times without flashing. Manual toolmaking built that stack by fitting one plate to the next: shim, scrape, spot, repeat. CNC toolmaking builds it by cutting every plate to the same coordinate system, so the fit is designed in the CAM file instead of discovered on the bench.

The practical difference shows up in three places. First, cavity and core geometry comes off a 3D model, so draft angles, radii and shutoff lands are consistent from the first cut. Second, plate pockets, guide-pin bores and ejector holes are drilled and bored in one setup, which keeps hole-to-cavity position tied to a single datum. Third, any change is a toolpath edit, not a bench decision.

None of that removes the toolmaker. It moves the skill earlier, into setup planning, stock allowance and inspection strategy. A shop that modernizes molds but keeps its old setup habits usually gets the same variation, just faster.

• 1
  Design intent survivesCavity, core and plate pockets share one coordinate system from CAM to CMM.
• 2
  Fewer bench decisionsShutoffs and parting lines are cut, not spotted by hand.
• 3
  Changes are re-cutA model revision becomes a toolpath revision.

A three-axis machine can cut most flat parting faces and simple pockets. Problems start when the cavity has deep ribs, steep walls or undercut shutoffs that a straight Z approach cannot reach without a long, thin tool. That is where 5-axis and 3+2 work pays off: the tool stays short and tilted, so it can reach a corner with less deflection and fewer electrodes.

Simultaneous 5-axis also lets a ball or barrel cutter stay tangent to a curved surface. On a deep draw cavity, that means fewer step-over marks and a surface that polishes faster. On the guide-pin bores and ejector plate holes, indexed 3+2 positioning keeps the bore round in one pass instead of two opposed setups.

It is not always worth it. A shallow, open cavity with generous radii and no undercuts is cheaper on a three-axis machine with a well-planned tool list. Adding a fourth or fifth axis only helps when the geometry, the reach or the number of setups demands it. GreatLight runs 16 simultaneous 5-axis centers, 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers, so the axis count is chosen from the part, not from what is free.

• 1
  Use 5-axis whenDeep ribs, undercut shutoffs, or reach that forces a long tool.
• 2
  Stay 3-axis whenOpen cavities, flat parting faces, generous internal radii.
• 3
  Rotary tableØ400 mm rotary table suits smaller inserts and core pins.

Most mold scrap is a datum problem, not a cutting problem. If the cavity insert is cut from one corner and the plate pocket is bored from another, the two features drift apart by whatever each setup carries. Modern practice is boring the guide-pin bores first, then using those bores as the datum for every later operation on that plate.

Stock allowance matters too. Roughing a 1.2343 or 1.2344 block leaves internal stress that moves the steel after it is cut. Common practice is to rough, leave 0.5–1.0 mm on critical faces, then finish after a stress-relief cycle. For a large insert, a second semi-finish pass at 0.2–0.3 mm removes the marks left by the roughing tool.

In-process probing closes the loop. A touch probe checks bore position and pocket depth before the part leaves the machine, so a shifted setup is caught while there is still material to correct it. That is cheaper than a rework route through EDM or welding. GreatLight inspects 100% before shipment, with raw material check, in-process monitoring and a final report on request.

• 1
  Datum firstBore the guide-pin holes, then reference everything to them.
• 2
  Stress reliefRough, relieve, then finish; leave 0.5–1.0 mm before finishing.
• 3
  Probe in cycleCheck bore position and depth before unclamping.

Mold steel is chosen from the plastic, the run length and the wear points. P20-type pre-hardened steel suits low to medium volume and cuts well on a 3-axis machine. 1.2343 and 1.2344 hot-work steels handle higher volumes and more abrasive fillers, but they arrive annealed and must be hardened after roughing, which reintroduces distortion.

That distortion is the reason heat treat sits inside the machining plan, not after it. Cut the rough cavity, send the insert for hardening, then finish-machine it in its hardened state. Finishing hardened steel is slower and needs a rigid setup, but it keeps the final geometry true. Hard milling at 45–52 HRC with small step-over is normal for shutoff faces and slide details.

Stainless and copper alloys appear where corrosion or thermal conductivity matters: 420 and 440C for corrosion-resistant inserts, beryllium copper for cores that must pull heat out of a hot spot quickly. Hardness, not price, should drive the choice. A soft insert that wears at the gate costs more in maintenance than a harder one costs up front.

• 1
  P20 classPre-hardened, good for low to medium volume, easy to machine.
• 2
  1.2343 / 1.2344Hardened after roughing; finish in the hardened state.
• 3
  Beryllium copperUsed for hot-spot cores where heat must move fast.

Cavity surface finish sets both the part appearance and how easily the mold releases. As-machined surfaces around Ra 1.6–3.2 μm are fine for hidden ribs and internal structure. Visible cosmetic faces usually need Ra 0.8–1.6 μm before polishing starts, and optical or transparent parts go finer. Fine finishing on GreatLight machines reaches Ra 0.2–0.8 μm.

The key point is that polishing removes material, so the machined surface must already sit slightly proud of the final form. Leaving 0.02–0.05 mm of polishing stock on a cavity wall is normal. If the machined wall is already at nominal, hand polishing will open the cavity and change the wall thickness.

Texture adds another layer. A VDI or MT grain is cut or etched into the surface, and the draft angle has to be increased to compensate for the drag the texture creates. Decide the texture before the cavity is finished, because adding draft after hardening is expensive.

• 1
  Leave polish stock0.02–0.05 mm on walls that will be hand polished.
• 2
  Cosmetic facesTarget Ra 0.8–1.6 μm before polishing begins.
• 3
  Texture and draftGrain adds drag; increase draft before finishing.

Modern mold machining is a capacity question as much as a technology question. Deep cavities need Z travel and spindle reach. Large plates need a table that holds them flat. Hard milling needs spindle torque at low speed and a thermally stable machine. A shop with one small VMC will hit a wall on anything above a certain insert size.

At GreatLight, three wholly-owned plants cover 7,600 m² with 127 high-precision CNC machines and 150 technicians. Travel options run from 4,000 × 400 × 150 mm for long, slim parts up to 750 × 1,150 × 550 mm and 600 × 600 × 600 mm for plate work. Maximum processing size is 4,000 mm. That spread matters because mold work rarely fits one envelope.

Materials handled include 6061, 7075 and ADC12 aluminium, 303, 304, 316, 420, 440C and 17-4PH stainless, 1018, 1045, 4130, 4140, 4340 and tool steel, plus C101, C110, beryllium copper and C36000 brass. Titanium grades TA1, TA2 and TC4, Inconel and magnesium AZ31B are also cut here.

None of this guarantees a good mold on its own. Machines, steel and inspection have to be planned as one system, and the planning starts at the DFM stage, not at the first cut.

• 1
  Envelope mattersCheck Z travel and table size before quoting a deep cavity.
• 2
  CertificationsISO 9001:2015, IATF 16949:2016, ISO 13485:2016, ISO 27001:2022.
• 3
  Quote speedQuotation and free DFM analysis within 12 hours.